Hi guys,

I tried to import a Mesh from CCM+ into Star-CD but after checking the cells I got error messages like cracks!

tried to make the mesh finner in ccm+ but didn't help - I tried to make couples in star-CD but am still getting error messages specially on the bends!

any help?

Hi,

crating couples in proSTAR is definitely sensless. ccm+ exports a polyhedral mesh without couples.

What do the areas around the cracks look like? I have seen similar things like concaves or centroid cells. In complex geometries ccm+ creates lots of them. However afer "remove invalid cells" ccm+ sometimes runs on the mesh... I think there is no chance to calculate such a mesh in v4.

Well, I tried not only polyhedral mesh but also Hexahedral cell as well but still getting all those error messages, crack and as you metioned centroid, concaves...

Creating couples in Star-CD is what support team at cd-adapco recommeneded me!

Creating couples is bullshit. All cells normally concerned in couples are polyhedral cells even if you generate a hexa (trimmed) or tetra mesh in ccm+ - the *.ccm format is a polyhedral format. You can check this by saying "cset news poly" in STAR v4 - this gives you all polyhedrals and you see that all these former couple areas (4 smal hexa faces to one large) have been replaced by polyhedral cells. (Large hexa gets one side with four small faces). There are two options: 1. Run in ccm+ (recommended) 2. Try to run in v4 as is

Are you sure these cracks are really cracks? Star-ccm exports your mesh with the unit meter, whereas in my opinion the default settings in Star-CD are more suitable for mm. My point is that you might not have cracks but small or thin neighbouring cells that are mistaken by the check tool for cracks.

Have a look at these areas in quick hidden view. If you have 'real' cracks you should see small internal walls.

Alternatively, have a look at the Delta value in the crack check tool. The default is 0.001, i.e. non-connected faces with a distance of 0.001 (m) or smaller are considered as cracks. check if you have cells in that size range and set the delta to a more appropriate value.

Hope that helps.

I suppose you are trying to do a multi-region mesh, for example, fluid/solid. If you use 1 mesh continuum in ccm+ and use poly meshing, export the ccm file and than merge the vertices's

cset all

vset news cset

vmerge vset,,,.00001 (tolerance)

If you setup multiple mesh continuums in ccm+, there is no guarantee you will get a 1-1 connection at the interface.